From: Chris Cheng <Chris.Cheng@xxxxxxxxxxxx>

Date: Tue, 10 Feb 2004 17:46:39 -0800

Steve & Ray,
Good point, there will be noise leaking out from the core through the
package. It will be "grossly inadequate" or attenuated to not affecting back
into other chips core through their package. So is this a matter of
containment or decoupling ? Like you said below, a nice faraday cage formed
by top and bottom ground planes stitched with ground via may just be as
effective as your decoupling solution.
Is it the wild Von Karmann wind that can knock the bridge off or the blow
that takes out the birthday cake candle ?
I believe it's just the later.
-----Original Message-----
From: steve weir [mailto:weirsp@xxxxxxxxxx]
Sent: Tuesday, February 10, 2004 2:13 PM
To: Chris.Cheng@xxxxxxxxxxxx; 'Istvan NOVAK'; Chris Cheng
Cc: si-list@xxxxxxxxxxxxx
Subject: Re: [SI-LIST] Re: Stack up for EMI reduction, plane resonance
and u-s trip radiation etc etc
Chris,
There is one point that I disagree on. Even though the package cuts off
with at least a -2 slope, there is quite of bit of high frequency energy
that still passes between the PWB and the IC. It is just grossly
inadequate to power the IC. But it has lots of potential to aggravate EMI
problems.
No one believed Von Karmann when he theorized that wind was the source of
energy that sent the Tacoma Narrows bridge into destructive
resonance. But, we all have learned that Von Karmann was right.
So now we have these resonant cavities in the form of PWB's with very low
damping coefficients. The IC's don't provide much damping, because as you
note the packages appear reactive, not resistive. As long as the energy
stays in the cavities and sloshes around at frequencies higher than the IC
cut-off(s), it probably isn't any big deal. But we have these: board
edges, vias, and components, all more than willing to provide radiation
paths for that energy.
One of the hotter debates was the 20H rule. Amidst that debate came the
notion of ground fences on the outside of the board. While I like those
for ESD, they can do just as much harm as good for EMI.
At 01:22 PM 2/10/2004 -0800, Chris Cheng wrote:
>Istvan,
>
>You got me on this one, I really need to figure out where can the
200-400MHz
>noise on PCB comes from ?
>Is it :
>a) Core noise, IC internal switch noise which propagate through the package
>power pins to the PCB
>Ans : Beaten to death, package is the choke point. EMI noise radiates from
>package not PCB
Agreed
>b) I/O switching noise, comes out from signal pins needs a return path the
>I/O power
>Ans : Managing the return path and reference plane not the decoupling caps.
>Yes, the plane CAPACITANCE not inductance provides the return path for the
>image current return through the opposite reference ground plane.
This is where as system integrators, we end-up applying band-aids due to
poor IC design.
Minor nit, I disagree with your characterization of plane
capacitance. Sure, without capacitance we would not have a coupling
mechanism, but at the frequencies of interest, the behavior over even
fairly short distances is of a transmission line, not a capacitor. This is
especially true with high K materials, and thin laminates.
>c) External terminators,
>Ans : The resistance of the terminator is the damping factor
Agreed.
>d) Noise from the supply
>Ans : 200-400MHz noise from a supply ??????
It's all those TWT's that they like to use in quarter bricks!!! ( Just
kidding, everyone knows it is the Klystrons. )
>e) External cable coupling
>Ans : ferrite beads and chokes
Moating near I/O, shunt devices such as feed-through caps, or X2Ys are
pretty effective too, adequate bonding of the PWB to the chassis, etc.
>Aside from the above, none of which is related to fancy decoupling caps or
>thin core PCB, where else ?
It is a matter of impedance. Either we get the decoupling capacitors
significantly closer to the package than lambda / 4, or we have stuck the
characteristic impedance of the planes between the IC and the caps. For
thick dielectric where that impedance can be an ohm or more, that is often
way too much. So, get close, or pay for fancy thin dielectrics.
What fancy decoupling capacitors can do is make it easier to stay close to
the IC by using fewer devices. But we are still stuck drilling enough via
holes to attach those devices.
Steve
>Chris
>
>-----Original Message-----
>From: Istvan NOVAK [mailto:istvan.novak@xxxxxxxxxxxxxxxx]
>Sent: Monday, February 09, 2004 7:58 PM
>To: Chris Cheng; si-list@xxxxxxxxxxxxx
>Subject: Re: [SI-LIST] Stack up for EMI reduction, plane resonance and
>u-strip radiation etc etc
>
>
>Chris,
>
>Well, it depends on the nature of the devil; if you are
>concerned by noise getting from the PCB into the
>package through its power/ground pins, you are
>correct: the package resonance will filter out noise
>above the cutoff frequency. If you also want to
>reduce the noise on the PCB itself, the active devices
>will not reduce the noise for the same reason, because
>the package separates the silicon from the PCB.
>
>Regarding parallel plate capacitance: this was discussed
>several times on the list, and I dont want to repeat
>myself. But I think we are saying the same thing.
>When you say parallel plate capacitance, I say
>inductance. For a board of a few inches in size or
>bigger, the lowest series resonance of the board plates
>is 100MHz or lower. Above that frequency the impedance
>is mostly inductive. If you need a certain amount of parallel
>plate capacitance, we like it or not, it comes with a certain
>amount of inductance above the series resonance. If
>you need more parallel plate capacitance, you get it
>together with lower inductance.
>
>Regards,
>
>Istvan Novak
>SUN Microsystems
>
>----- Original Message -----
>From: "Chris Cheng" <Chris.Cheng@xxxxxxxxxxxx>
>To: "'Istvan NOVAK'" <istvan.novak@xxxxxxxxxxxxxxxx>; "Chris Cheng"
><Chris.Cheng@xxxxxxxxxxxx>; <si-list@xxxxxxxxxxxxx>
>Sent: Monday, February 09, 2004 4:33 PM
>Subject: RE: [SI-LIST] Stack up for EMI reduction, plane resonance and
>u-strip radiation etc etc
>
>
> > Yes, once again the devil is in the details. It is one thing to stick an
> > impedance probe to measure the power plane impedance at a random
location
>on
> > the PCB. It is another thing to measure it on the real load side (i.e.
>after
> > the package). Have you done that ? Are you convince you can even see any
> > effect at 200-400MHz on PCB through the package ? Your colleague Larry
and
> > me don't think so.
> > As for I/O return current related noise on PCB, it is the parallel plate
> > capacitance that sandwich the stripline which is responsible for the
> > decoupling/return of the current (at least at 200-400MHz). Not the thin
>core
> > power/gnd pairs or fancy decoupling caps.
> >
> > -----Original Message-----
> > From: Istvan NOVAK [mailto:istvan.novak@xxxxxxxxxxxxxxxx]
> > Sent: Sunday, February 08, 2004 3:07 PM
> > To: Chris.Cheng@xxxxxxxxxxxx; si-list@xxxxxxxxxxxxx
> > Subject: Re: [SI-LIST] Stack up for EMI reduction, plane resonance and
> > u-strip radiation etc etc
> >
> >
> > Chris,
> >
> > I am not speaking for Zhangkun, but in many of the real boards I have
>looked
> > at by measurements and simulation, you can see the evidence of
>antiresonance
> > between the plane capacitance and inductances of capacitors. Chips (at
> > least on those boards I have looked at) did SHIFT the resonance
frequency
> > slightly, but did not make the peak go away. You are correct in saying
>that
> > if you sprinkle the board with capacitors, the resonance peak is
>suppressed.
> > But as you said in one of your recent postings, the devil is in the
>details:
> > sometimes you may need so MANY capacitors over the board area to
> > sufficiently suppress the resonance that it becomes a pain.
> >
> > Regards,
> >
> > Istvan Novak
> > SUN Microsystems
> >
> > ----- Original Message -----
> > From: "Chris Cheng" <Chris.Cheng@xxxxxxxxxxxx>
> > To: <si-list@xxxxxxxxxxxxx>
> > Sent: Monday, February 02, 2004 10:15 PM
> > Subject: [SI-LIST] Stack up for EMI reduction, plane resonance and
u-strip
> > radiation etc etc
> >
> >
> > > Finally......
> > >
> > > Zhangkun,
> > >
> > > I am also curious about these 200-400MHz plane resonace. If you
sprinkle
>a
> > > PCB with a wide range of caps with different values and at different
> > > location and with high power loading (ie real IC chips) at different
> > > location, do you still see pronounced peaks at 200-400MHz ? I have no
> > doubt
> > > a bare power/gnd plane pair can resonate at those frequencies, but
I've
> > > never seen that case once realistic caps and loading (IC chips) is
>placed
> > on
> > > the PCB. Are these simulation results or measurements based on a real
> > system
> > > with chips and caps ?
> > >
> >
> >
>------------------------------------------------------------------
>To unsubscribe from si-list:
>si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
>
>or to administer your membership from a web page, go to:
>http://www.freelists.org/webpage/si-list
>
>For help:
>si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>
>List technical documents are available at:
> http://www.si-list.org
>
>List archives are viewable at:
> http://www.freelists.org/archives/si-list
>or at our remote archives:
> http://groups.yahoo.com/group/si-list/messages
>Old (prior to June 6, 2001) list archives are viewable at:
> http://www.qsl.net/wb6tpu
>
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
http://www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List technical documents are available at:
http://www.si-list.org
List archives are viewable at:
http://www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu